Drill Recomendation

[robk]

The material being cut is In-100 (pretty nasty nickel based alloy).

Currently using a Titex drill (A6489DPP-9.2) @ 53 sfm @ .003 ipr with life of only about 20 holes but we need to machine 28 per part (we have played with speeds and feeds and so far these are our best results we were able to achieve- They are almost exactly what they recommend as well, but according to Titex we should be able to cut 70 holes). We have tried the drill with coolant as well as oil with pretty similar results. This process will be locked so once the tools as well as the speeds and feeds are selected there is no way of changing them without cutting up the part again.

The holes are only about .300" deep and the process includes 140° spot drill since the holes are on a concave surface. The drill must stick out a minimum of 3.5" inches because of side clearance issues.

We will most likely try to sticking with oil, so no coolant through is needed. Looking at the 3 flute Garr drills series 1100H, but would also like to hear other manufacturer suggestions for solid carbide drills with above said minimum stickout and Ø.359-.362 range.

[RaiderX]

if possible choke that drill or a stub up in an extension holder and no spot. my guess would be it is wearing corners on entry? have had pretty good luck with guhring drills. drilling can be a nasty op in tough materials, lots of variables to consider.

[robk]

_{I have only about .05" max clearance per side @ 3.3" stickout so the stickout needs to be what I originally posted. As I mentioned above the surface is concave on an ID of a hub so without spotting I would be hitting with the corners 1st. I am using 140° spot drill.}

_{We have done a few different variations of this part before, but they keep on changing the design and it just keeps on getting more complicated.}

_{I will take a look @ what Guhring has to offer.}

 

_{Sorry but that's the most I could show}

[?Mark]

It seems (at least in my experience) that spotting in tough materials tended to change/HT the surface of the entry hole. Something that I found worked in extending the life of a carbide drill is to mill a flat just a few thou bigger than a hole, center drill a point if necessary, drill it and than add a chamfer...

Titex, prototype (sp?), mitsubishi, sumitomo, guhring and iscar are my fave brands for tough material drilling.

 

You got some tough stuff there Rob

 

Edit:

Just saw a picture...milling a flat is a no-go.

Using 2 spot drills? 1st to rough and 2nd to finish?

Tough...

[robk]

^{Hi Mark}

^{On the previous versions of this part (and there was @ least 1/2 dozen already with each one being different) we had no issues. We either drilled the holes or helically interpolated them, but the clearances were a lot more friendly. This one kind of limits us a bit as to what we could do. Thanks for your input.}

[SledGeek]

I have really good luck with Sumitomo GS series . I usually use GS4's (4x dia) and they love aggressive cutting in hard, tough and gummy materials. Typically run them in the 120-160 sfm range with anything from .004-.006.......

[GoetzInd]

We've had pretty good luck with Widia vari drills and TopS drills in Ti's and SS. We also have had good luck w/ titex though. Why do you say the process will be locked? Is this an AS requirement or is it your customers/internal?

This process will be locked so once the tools as well as the speeds and feeds are selected there is no way of changing them without cutting up the part again.

 

How hard of a time are you having coring it out and turning it?

 

Mike

[robk]

^{We have a lot of jobs in here that are PWA ESA (Engineering Source Approval) where the customer requires us to lock the process once it is proven. Usualy critical parts as well as rotating parts require this process (as we speak, I believe that Pratt is investigating a part that has a crack in it for the JSF). The parts get cut up and checked with a fine tooth comb. Not just the tooling that has to get locked, but the machines as well. So no changes at all without the customer's approval. Can't run the part on a different machine (can't even move the machine to a different location---gonna be fun with our move to the new facility!!), can't use a different coolant, or tools, can't play with speeds and feeds, can't run the cutter longer then it was proven for, no regrinds, etc...}

^{I did not do any of the turning programs for this part, but I think they have gotten through the cut-up by now. I know there is a lot of trochoidal paths to get into the deeper grooves, but this part is no different for what we normaly do. It'sthe paperwork takes even longer tan non ESA parts. Better make sure every I is dotted and T is crossed. A lot of autographs that I have to give with those jobs as well.}

[robk]

BTW, I am having a few different brands dropped off next week for try outs. Requirement will be 1 drill per part (Titex are about $140 each) and with hi production order everyone is willing to give a tool for free to make sure they get the order.

I'm off to Bike Week in Daytona Beach tomorrow, so I'm out of here early today.

Later

[DavidB]

I would try reducing the feed rate at the entry to 50% until the full diameter of the drill has reached the lowest point of your concave surface. Then increase feed to 100%.

I assume you are not pecking.

 

What is the positional tolerance of the holes?

[DavidSV]

At those costs and yields, why don't you just have a company like Guhring make you a special drill. It could be larger on the shank to where it almost rubs and then ground down to the drill diameter on the tip. If you have enought quantity, you can just have them made as a production run of drills and order them in larger batches.